Click Geometrical Tolerance
in the Dimensioning toolbar (Tolerancing
Select an element (geometry, dimension, dimension value,
text or point) or click in the free space to position the anchor point of
the geometrical tolerance.
If you select an element, the anchor point will be an
arrow. Note that you can modify this symbol by
editing the annotation leader.
If you select a point in the free space, the anchor
point will be a small balloon.
If you select a dimension, the anchor point will be at
the intersection of the dimension line and the extension line.
If you press the Shift key and select the extension
line, the leader is perpendicular to the extension line and the anchor
point corresponds to the position of the cursor when you click to
create the geometrical tolerance.
If you select a dimension value or a text, no leader
will be created. The geometric tolerance will be displayed just below
and parallel to the element you selected.
Move the cursor to position the geometrical tolerance and
then click at the chosen location. The Geometrical Tolerance
dialog box appears.
- At this step, you can apply the parameter values of an existing
geometric tolerance to the tolerance you are creating: to do this,
simply select the existing geometric tolerance.
- If you have selected the Use style values to create new
objects check box in Tools > Options > Mechanical Design
> Drafting > Administration tab, the Geometrical
Tolerance dialog box is pre-filled with custom style values
(as defined in the Standards Editor). In this case, Properties
toolbars and the Tools Palette are disabled during the
creation of the geometrical tolerance.
On the other hand, if you have not selected this option, the
Geometrical Tolerance dialog box is pre-filled with the last
entered values (if any). In this case, Properties
toolbars and the Tools Palette are active during the
creation of the geometrical tolerance.
- You can reset the current style values in the Geometrical
Tolerance dialog box at any time using the Reset
Select the Filter Symbol check box to filter
the available tolerance symbols according to the type of geometrical
element you selected (if any).
||If you did not select any geometrical element, the tolerance
symbols will not filtered.
Specify the tolerance type by clicking the Tolerance
Symbol button and selecting the appropriate symbol.
Type the tolerance value in the Tolerance
value field, adding symbols as needed. To do this, position the cursor at
the proper location in the field, and click the Insert Symbol
button to choose the appropriate symbol.
||You can add symbols to the tolerance and reference value as well
as to the upper and lower text.
Type the reference values in the Reference
value fields, adding symbols as needed.
To add a new geometrical tolerance, click the Next line
arrow button and repeat steps 4 to 5.
Type the upper and lower texts in the appropriate fields.
You may also add symbols if you want to.
The geometric tolerance is updated as you define values
for each field.
Click OK when you're done. The geometrical
tolerance is created.
You can add an all-around symbol to the leader. To do
this, select the geometrical tolerance, right-click the yellow
manipulator on the arrow and select All Around from the contextual menu.
Specifying Leader Orientation
You can orient the geometrical tolerance leader perpendicularly to the
element to which it is associated (for example, if the leader is associated
to a dimension, you can position the leader parallel to the dimension line
and orthogonal to the extension line).
For this, you have two different possibilities:
- Either go to Tools > Options > Mechanical Design > Drafting >
Annotation and Dress-up tab and check Snap by
toggles). Then, click the Configure snapping button and select
either On orientation or Both. To orient
directly the geometrical tolerance leader perpendicularly to the
associated element, press the Shift key before clicking in the
drawing to position the tolerance (see previous scenario, step 3).
- Or go to Tools > Options > Mechanical Design > Drafting >
Annotation and Dress-up tab and check Geometrical tolerance
in Annotation Creation. The leader will be oriented
perpendicularly to the geometry by default. In this case, pressing the
Shift key will let you orient it differently.